Proma THC makes Masso go crazy. (PROBLEM SOLVED WITH A BUG FIX)

[Ross]

Yes I am still having problems with this!

(1) Still getting soft limit errors on the Z axis when the Proma has power to it, even in test mode doing a dummy cut, every time it does a touch off it adds extra amount to the Z machine position till it finally Z's out.

(2) In real life running plasma plus thc, doing a 90mm line test off 6 lines, it just cuts one line go to the next start point then give a "no ark ok signal"

error.

(3) In real life running plasma plus thc, doing a 90mm line test off 6 lines, it cuts two lines stops then give a "no ark ok signal or soft limit error"

(This only happens when the Proma has power to it).

Just don't have a clue now.

I really need to sort this out cause I have been fighting with for too long now.

From Ross.

Cut File attached.

 

[jolbas]

I have had similar issues when THC is active but I never found a G-code that reproduces the problem. It happens now and then. Less often now than when I started using my machine in October. I have made a lot of adjustments to my post processor during this time so maybe some of the changes did prevent it from happening. One change I did (because of another issue) was to turn on and off my THC using M62 and M63 instead of using M667 and M666. And I don't turn on and off my THC during feed. I would like to but I risk to run the nozzle into the material. And also I don't trust the modality of G1 and G0 so I start every row feed or rapid move with a G0,G1,G2 or G3. I can't find any recommendation on G-code style for Masso in the documentation. Would really like some notes about a preferable code structure. i.g

If I look at your G-code I would suggest changing

N0190 G01
N0200 M667 F400 (---THC on---)
N0210 Y90.0000 F2400.0

to

N0190 M667 F400 (---THC on---)
N0200 G01 Y90.0000 F2400.0

I at least would prefer it if I was Masso.

Regards

/Bj rn

 

[jolbas]

I also have another hypothesis about this issue that I have not yet investigated. I think I sometimes have sent too high pulse rate to my Z stepper driver. It seems to lose track at about 20 kHz.

This does not depend on if THC is active or not but should affect probing cycles where you have G0 commands on Z.

 

[jolbas]

Is it possible that Masso loses some of it s pulse rate capabilities if it has to keep track of THC signals? Try to lower the maximum speed on Z axis or reduce the amount of microsteps.

 

[Ross]

Thanks Jolbes,

I just got back from the parents house out in the village and will make these changers to see if it works.

The G-code looks nearly the same as mach3, so I will try to change the postscript.

Will drop the feeds by half as well and see what happens.

Still not sure if I still have electrical noise but I have shielded all the wiring, something else to go through again.

Thanks From Ross.

 

[jcoldon]

Ross most likely it your wiring all inputs homing and torch touch should be NC 24 v shield wire.. The torch touch switch you might need to isolate it... if your running 5 volst the stupid pull-up resistors might be causing a voltage drop

The masso guys are not plasma guys they are mill and router guys

What lacking is THC controls on the screen they relying on g codes from sheet cam

All sheet cam does is cut height and pierce height and feed rate pierce delay unless you want to build some custom post then you got go in there to make changes it needs max and min THC height .ignition height for when your pierce height is higher thc on delay and a setting to keep the thc from moving the z apron start like a reference voltage setting and a speed reaction setting ON THE SCREEN this all needs to be in the masso screen until they build an integrated THC the thc will never run right it lacks control it will work just not good

Example thc on your voltage spikes z moves to correct it torch rises with out a max setting it going to go way up same thing for down anti dive is another it try to make a voltage correction rams the torch in the table the proma is a simple device that reads voltage whatever you set it at it sends up down closers to move the z with a change to correct the reading. Nothing else

The plasma process it lower torch HIS switch active torch rises to pierce height.. Torch ignites pierce delay starts then cut height.. Then THC takes over cut.

So were the min max setting and anti-dive and ignition height in the masso

A simple delay setting on the screen would be good for when the pierce setting completes and cut height starts there a timer setting for THC delayed inputs this way voltage will settle on cut start before THC

The rest of the unit is fine this is a plasma masso why they haven t made it plasma and put in a good THC and add the controls needed for plasma I even pay extra for a good integrated THC and ohmic touch

And make a second input for ohmic to you can run either or

 

[masso-support]

There can be multiple issues and as mentioned @jolbas lets first check if its not due to too high feed rate or acceleration.

@ross when you get an error on Z axis, can you please move (JOG) the Z axis up all the way and check that the Z axis position is at the same location where the machine is homed and the machine coordinates on the screen show the same homing position.

 

[Ross]

Hi Masso, I have The THC feed rate at 400mm min and jog feed rate at 250mm min.

The torch touch off Zeros the machine on the first cut then the machine Z position changes every time on the second cut like it has a mind of it's own.

After I get the Z error it will only jog part of the way up, some times the whole way up.

I normally power off then power on and home the machine to do a new test.

Photos: 1A and 1B is from yesterday and shows coordinates of machine and where the plasma cutter stopped.

Photos 2A and 2B is todays attempt and shows coordinates of machine and where the plasma cutter stopped about 6mm above the job.

Tap line test is from today.

Thanks in advance from Ross.

------------------------------------------

jcoldon: I am using 19volts from an old laptop to power the Proma and lowered the feed speeds for this test,

Thank you for your help from Ross.

 

[masso-support]

thanks @ross but still not clear about the issue.

In the first test can you write a program that you dont turn on the plasma and follow these steps:

1. Change the same program so that the plasma is not switched on or off.
   
2. After homing the machine, move the Z all the way up and I think it will be your machine Z 0.00 at that point. Mark this point with something so that you know where your Z 0.00 is after homing.
   
3. Run the program and after it has touched the metal a few time (5 to 10 times) using the G38.2 cycle, move the Z axis to machine Z 0.00 (not work Z0.00)
   
4. Now check if this matches the previously marked Z 0.00 position and let us know.
   

 

[Ross]

Hi Masso,

I made two files today.

The file with M03 and M05 removed worked fine machine Z was good.

The file with M03 and M05 not good, machine Z values changed from -43.069mm to -71.541mm over the course off twenty lines.

Have two photos showing work position while traveling part of the way on first line and last line so you can see the machine reference on the bad one.

Plus the two tap files.

Thank you for your time. from Ross.

 

[masso-support]

so with the 20-lines-No-plasma.tap file did the Z axis moved down and touched during the entire program run?

 

[Ross]

Hi Masso,

20-lines-No-plasma.tap file did the Z axis moved down and touched during the entire program run? "YES."

20-lines.tap has the problem it does the full run but looses machine coordinates.

Video shows the problem

Thanks from Ross.

 

[testyourdesign]

Hi @ross

This problem appears similar to the Ctl J Line Jump error they found before the last update. Masso would get lost when ever a temporary work offset (G92) was used. From looking at your video I see that you are in G92 mode so you must have zeroed the DRO's to get it that way. Maybe you should try setting the work offset using G54 instead so that you can see if its a bug with G92.

To do that you need to

1. Enter G92.1 in MDI to change over to G54 mode
   
2. Then Jog the over to the location you want to start cutting.
   
3. Switch over to work offset page and double click on G54.
   
4. Autoload the current X, Y and Z position of the torch.
   
5. Edit the G-Code to include G54 at the start of the program.
   
6. Re-run to see if the temporary offset caused the problem.
   

Hope this helps.

Cheers, Stephen Brown

 

[Ross]

Sorry Stephen it didn't help.

The issue is to do with the "F1 screen Proma THC 150" combined with the M03 and M05 codes that turn the plasma on and off.

It will cut fine with "no plasma ok signal and THC" set from F1 screen. but that means when the sheet warps from heat the torch will collide with the job.

From Ross.

 

[masso-support]

thanks for the video @ross and will setup to run our machine exactly as per your setup and will get back to you.

 

[masso-support]

@ross, we were able to replicate the issue with 20-lines.tap whereas 20-lines-No-plasma.tap ran fine and yes it's not the issue with the steps being lost on the Z stepper.

we have set the priority of the bug fix to HIGH and will be working on this on priority.

 

[masso-support]

@ross we found the issue and its a mix of a few things. Please see the below:

1. Firstly please note that the delay value for G04 is in milliseconds, P0.5 will be only 1/2 millisecond. For 1/2 second delay please use P500
   
2. When THC mode is enabled using M667 the UP/DOWN signals move the Z axis.
   
3. At this stage Z axis should not be moved using gcode and only any Z axis movement issued after disabling THC using M666
   
4. What is happening is that the gcode is switching on THC and then also giving command to move the Z axis, the controller is then trying to move the Z axis with gode and also with input signals from PROMA.
   

Fix:

1. On our side we are adding logic that if THC mode is one then Z axis movement via gcode or JOG will be ignored, this will act as a safeguard that if Z is tried to be moved when THC on the system will not get confused.
   
2. The gcode should follow this sequence:
   1. goto X, Y position
      
   2. move Z axis to do a touch using G38.2
      
   3. move Z to piercing height
      
   4. start plasma using M3
      
   5. move Z to cutting height
      
   6. switch on THC using M667
      
   7. cut material using any X and Y movements.
      
   8. switch of THC mode using M666
      
   9. switch of plasma using M5
      
   
   
   

 

[Ross]

Thanks for the reply,

I had changed the Masso post script in the past in Sheetcam to seconds will change it back to original to save confusion on your side, if I need to send tap files to you in the future.

Ok; To upgrade the fix will it be updated in your website under CAM Post Processors,

or just sending an email to me just for the logic update?

Once I have done the upgrade and changers I will do more test cuts and get back to you with the results.

Thanks again for your help from Ross.

 

[jcoldon]

I looking at this whole post this is a mess you should be able to make cuts with no thc first off... the cuts are not good lots of waves in there possible bad gearing

You cut high wrong lots of dross. Does all the measured movement match your dro? Don t use to high of a micro step setting in your motor driver Or your goanna miss steps... I built several tables and have a lot of people using my designs I do know this stuff. I purchased a masso getting ready to use it on table 3 for someone but from what I see the THC or it screen controls are not there yet. masso has a way to go. But seems to think let s put every control in the g code. currently I run mach 4 with a vital systems controller and there plasma screen... I thought I give masso a try save some people money on controller builds and no pc... it seems they have a long way to fix there THC controls and how it interacts with the cutting process . Don t get me wrong I not putting the controller down it just without THC plasma cutters ar no good. I also purchased an external step direction the from robot 3t I figured the masso the was not ready yet

How does a masso prevent the THC from rising to high or going to low drive the torch in the table there no min max settings for THC? I like to see masso do some features like the my cnc software has in it for their thc very nice cut algorithm in it. or have features like the nuron unit .

Fix the THC make in integrated read the voltages fast response and small table OEM will use the controller I knew this when I purchased the controller last year they told me I figured I prove the oem wrong. I figured masso buy know would have fixed there THC all they did was throw a gcode to have a separate z THC speed. Well if your goanna have separate plasma controller it should work like one.

Ross trie running squares... and stars. Triangles.. That way you can see if things are running right then move to circles. lines you don t really need... weight the metal down an old car roter works good .Run cuts with no THC get it all dialed in then when all is good then use the THC otherwise you drive yourself batty lol. Everything should run good with no THC if not fix it your almost there

 

[masso-support]

the updated post will be helpful for sure @ross and we will upload the new one to our site.

We are working on the software changes on MASSO and will email you the software when ready but in the time being you should be able to run the current software version of MASSO with gcode changes.